Separation contact not working

[leongkokheng]

Hi,

I'm trying snap fit analysis using Nastran In CAD 2018.

I've tried Non Linear Static with Large and Small displacement options.

However, the separation contact that i created manually is always having penetration.

I also attached the Inventor files here.

Please advice.

Thank you in advance.

[John_Holtz · Accepted solution]

Hi @leongkokheng

Your parts penetrate because you told the software to delete the contact elements if the part moves more than 0.1 mm, and the parts need to move 4 or 5 mm before they come into contact!

In other words, the "Max Activation Distance" on the contact dialog is a filter: contact elements that are shorter than that distance between nodes at time 0 are created; elements that are long are not created. If the contact elements do not exist between pairs of nodes that "come into contact", then there will be no contact detected.

So, the changes that I made to the contact setup are as follows:

1. The "Max Activation Distance" needs to be 10 mm (or slightly larger) since the parts are moving 10 mm.
2. I was getting some penetration which indicated that the "Stiffness Factor" was too low. So I tried a value of 0.3.
3. I like to use a "Penetration Surface Offset" value other than 0. By using a nonzero value (such as 0.09 mm), contact occurs before the parts pass through each other. If desired, the stiffness factor can then be tweaked so that the parts just come into contact.

I also changed the Nonlinear Setup > Advanced so that the model was easier to converge. I noticed that the analysis (on one of the timesteps) had converged on displacement and work but not on force. You really do not need all 3 since work incorporates force. See the attached images.

Edit: I almost forgot to mention that the analysis with these changes got to 99% complete before it said that it could not converge. No doubt you can make a small change to any of the input (such as the stiffness factor or even the distance of the enforced motion) and get the analysis to complete.

[John_Holtz]

Hi @leongkokheng

I wanted to see if you have any questions about the contact analysis.

I did find this article that describes the maximum activation distance. It might help to explain what that input does. See Understanding maximum activation distance and contact type in a Simulation

Take  your time (of course), but due to time zone differences and upcoming holidays, you may not receive a reply until Wednesday if you wait until after Friday to ask any questions. (I am in the same time zone as New York in the United States, and Monday is a holiday).

[leongkokheng]

Hi John,

Thank you for your explanation. I thought the Maximum Activation Distance will be updated for every incremental steps. That is the reason why I set a small value for it. Now, I understood that this is the value that the software use at the beginning of the analysis.

Alternative solution

I moved the parts closer to each other (separation distance is less than 0.5mm).

I changed the analysis to Nonlinear Static.

I use the following settings for contact surfaces. I activated the Maximum Activation Distance but did not enter any values.

With these settings, I managed to get the surface contact activated between 2 parts:

Thank you.

[Anonymous]

---

@leongkokheng wrote:

Hi John,

Thank you for your explanation. I thought the Maximum Activation Distance will be updated for every incremental steps. That is the reason why I set a small value for it. Now, I understood that this is the value that the software use at the beginning of the analysis.

Alternative solution

I moved the parts closer to each other (separation distance is less than 0.5mm).

I changed the analysis to Nonlinear Static.

I use the following settings for contact surfaces. I activated the Maximum Activation Distance but did not enter any values.

With these settings, I managed to get the surface contact activated between 2 parts:

Thank you.

Hello all,

I am new here and try also this simulation. I see that your simulation work. Can you upload your file again with your solution please?

Thanks

---

[leongkokheng]

Hi,

Good day!!

Please find the attached Inventor 2019 files from here.

All the settings are done. You just need to re-run the analysis using Nastran InCAD.

Hope this helps.

[jgomezKRRHB]

Dear leongkokheng,

I am having a similar issue with a separation contact not working as expected. I downloaded and ran your example but I didn't get results similar to the clip of your post. Can you check whether it was the right file or not, please?

Thanks in advance.

Jose Gomez

[leongkokheng]

Hi Jose Gomez,

Good day!!
I download the zip file and just click Analyze. No need to re-mesh or do anything.

Can you tell me what is not working?

Thanks.

BR,

Kok Heng

[jgomezKRRHB]

Hi Kok Heng,

It was a proble of deformation scaling. If you use the default settings it looks like the contact is not working, so I changed to a smaller scale.

Thanks for your interest and help.

Regards,

Jose